Hey guys.
I just want to know that how can i find the speed and feed rates for drilland tap tools.
because everytime i use mastercam default speed and feed it causes me to break the tool..
so if any feedback would be most appreciable.
i have the foolowing tools
17.5mm,15.5,14.0,12,10.2,8.5,6.8,5,4.3,3.4,2.6 and all are hy-pro coolant drills
M20*2.5, M18*2.5, m16*2.0, m14*2.0, m12*1.75, M10*1.5 all are hy-pro coolant taps
i just wanted to know the exact feed and speed rate for this tools in inches.
thanks in advance..

First Mastercams Feeds and Speeds are based on how you set your material up, either alum, steel, etc. No one that I know uses the default settings.

Most people create their own custom tool libraries with their own feeds/speeds. Etc, a library for alum, steel, stainless, etc. Then you just select the library based on the material you are using.

I am lazy, I just customize the tools that are in there by selecting a tool when I program, change the feeds/speeds when I program in the tool definition then save that tool to the library, then it will be there the next time.

As far as what you should run your tools at, the product literature is always where I start. Especially for your tools, you should always start with the manufacturers recommended speeds/feeds. Normally their sites have this literature or contact your tool salesman, he should help you.

Taps are a bugger all the time. I normally always run them with a feed of F10., back figure the spindle speed based on pitch. For metric stuff I try to figure out the best round configuration between F10. and F20., because it doesn't work perfectly with the pitch. If you don't want to run a tap slow, then I would also say look to the literature for it.

My motto is, my tap slow, but a slow tapped hole that doesn't break the tap, is better than breaking a $50 tap and then having to dig it out with a couple endmills too.

*** Spindle Speed / thread per inch = feed per inch
*** feed per inch * thread per inch = Spindle speed
Metric taps have pitch, so depending if your machine uses Feed per Inch or Feed per Rev you need to convert.
1(inch) / threads per inch = pitch
1(inch) / pitch = thread per inch
hope something here helps.

cncmike


cncmike

Thanks Mike, i really appreciated your help.
Actually our company just drills and tap holes on Stainless steel, Carbon and mild steel.
we have a manual here but it just says something like this
Stainless steel 300ss, 400ss
cutting speed for stainless is 120-180 SFM.
so what cutting spped can i take for any drill that i have listed above..
confused with that stuff.
one more thing man you just rock.......
thanks.

SFM means surface footage, in machining terms...

SFM x 3.82 / diameter = RPM

so if you have a 17.5mm drill

17.5/25.4 = .6889" diameter (convert metric to inches)

Take your 120 SFM(the low side)

(120 x 3.82) / .6889 = RPM

458.4 /.6889 = RPM

704 RPM

Then to find your feed rate it's----

RPM x chip load(per tooth) x teeth(flutes) = feed rate(inches per minute)

If you use your 704 RPM from the example

704 x chip load(per tooth) x 2 = feed rate(inches per minute)

Not knowing what the recommend chip load is, but I will use .001" per tooth for an example

704 x .001 x 2 = F1.4(inches per minute)

**Note alot of drill manufactures may say inches per revolution, if that's the case ---

RPM x chip load(inch per rev) = Feedrate

*** Note these are standard formulas in machining, 3.82 is a constant for all machining, example to find RPM for endmills, drills, taps, indexable tooling, even for turning, you would use your diameter of your part you are turning to then.

hope it helps,

cncmike

Good starting points:
http://www.techsolve.org/manufacturing/ ... -handbook/
(You can search for "Machining Data Handbook" too).
http://www.cutdata.com/

Always think in terms of SFM & IPT or IPR.

jbtech

Thanks mike.........
I appreciate the things that you told me and i calculated with the lowest rates.
so finally i will be trying out these speed and feeds today.
one more thing is that can you tell me how to chamfer in mastercam.
i want to chamfer a drill hole of 12mm.
thanks a lot again.

Thanks jbtech i saw all the webpages you posted but they all tell to buy these books from them...

Hey Mike are this speeds and feeds ok
i just calculated by your method.
Drills Speed Feeds
M17.5 704 7.744
M15.5 751 8.263
M14 830 8.307
M12 970.36 8.733
M10.2 1141.43 9.131
M8.5 1369.58 9.58

Welcome, I use the same drills and taps from OSG. If you look in there master catalog or on line, OSG provides the chart for recommended RPM and feed per rev. In this case you would take RPM x FPR = IPM. Note that the feed for coolant feed drills are more aggressive. When drilling a deep hole say 5 time OD of drill I use a peck of 35% to 25%. However in most cases with coolant feed drills you will not peck as long as enough coolant pressure is there to clear the flutes of chips. The chart is in a PDF form on line that you may down load to create your tool file from.
As far as Master Cam is concerned I have also created my own tool library based upon materials for these tools. I too am lazy as well and do not like reinventing wheel each time I post a program so I use my own tool files to insure correct feeds and speeds are posted. It take a little time to set up, but save a lot of time and headaches later on.

Hey Kenneth D Ramsey JR.
I was wondering if you can give me the feed rates and speeds for all the drills and taps from osg.
in the above post i have mentioned the hy pro drills .
please if u can or attach a file so i can download that file.
Actually we bought a brothers machining center and the tools are breaking one by one, see if u can give me Taps feed and speed too.
http://www.osgtool.com/HY-PRO®DIN-c269.html, i use all of these tools.
Thanks for your help.